Recutting single point threads

All things related to the Centroid Acorn CNC Controller

Moderator: cnckeith

Post Reply
ScotY
Posts: 654
Joined: Sat Sep 23, 2017 7:57 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: none
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
Location: Honolulu, HI

Recutting single point threads

Post by ScotY »

Is there a way to single point thread and then go back and thread it again but cut deeper threads on the next run?

I saw CNCKeith’s video where he did some threading, moved the spindle around and reran the program and it ran perfectly without damaging the existing threads. My question would involve editing the gcode or, preferably, editing the file using Intercon. So, as that is not the same thing, I’m not really sure if this will work? The encoder knows the position of the spindle but if you run a new (or edited) program, I would think it would disregard the known position?
frijoli
Posts: 595
Joined: Tue Sep 12, 2017 10:03 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 1030090099
DC3IOB: Yes
CNC12: Yes
CNC11: Yes
CPU10 or CPU7: No
Location: Outside Winston-Salem, NC
Contact:

Re: Recutting single point threads

Post by frijoli »

ScotY wrote: Tue Feb 06, 2018 3:30 am Is there a way to single point thread and then go back and thread it again but cut deeper threads on the next run?

I saw CNCKeith’s video where he did some threading, moved the spindle around and reran the program and it ran perfectly without damaging the existing threads. My question would involve editing the gcode or, preferably, editing the file using Intercon. So, as that is not the same thing, I’m not really sure if this will work? The encoder knows the position of the spindle but if you run a new (or edited) program, I would think it would disregard the known position?
Yes you can, as long as you do NOT move the part in the chuck/collet, and you don't change the Z position in the file. This has been my experience with all machine tools.I have not tested this in a Centroid machine, but If you don't change the start of the thread it should always start at the same point. You can actually see this in the G code file before you attempt it.
Write the Intercon program, look at the start of the thread in X and Z, then modify the file for the start and finish diameter. Post and look at the start in X/Z.
Pretty straight forward to confirm.

Obviously you cannot change the pitch.

Clay
Clay
near Winston-Salem, NC
unofficial ACORN fb group https://www.facebook.com/groups/897054597120437/
rl49
Posts: 52
Joined: Wed Nov 23, 2011 11:04 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: K2019,K1110
DC3IOB: No
CNC11: No
CPU10 or CPU7: Yes
Location: Finger Lakes, NY

Re: Recutting single point threads

Post by rl49 »

we have a T400 and just adjust the wear offset to cut deeper no modifying any files intercon or posted gcode, works excellent for fitting gun barrels to receivers right on the lathe

Ron
cnc_smith
Posts: 237
Joined: Mon Nov 20, 2017 10:13 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: none
DC3IOB: No
CNC11: Yes
CPU10 or CPU7: Yes
Location: Frenchville, PA

Re: Recutting single point threads

Post by cnc_smith »

For threading cutting if the mating part does not fit all you have to do for an OD thread is use the Tool Wear offset and offset down (negative direction) to adjust to get the part or thread gage to go. For an ID thread offset up (positive direction). If you change the program starting Z the threads will be ruined if you try to re-cut the same part. You can change the ending Z in the program to cut the thread longer or shorter and that will not effect the thread. The control keeps tract of the spindle encoder and the Z positions for starting position. Re-posting the program will not effect the thread as long as the Z start position and/or in Intercon the Thread Angle is not changed . If the control is homed to reference marks and the machine is powered down you will not be able to re-cut the threads on that same part. The lathe in the video homes to switches that are a plunger type that are very repeatable.
Dana

When requesting support, please ALWAYS post a current report.
Need support? READ THIS POST first. http://centroidcncforum.com/viewtopic.php?f=60&t=1043
All Acorn Documentation is located here: viewtopic.php?f=60&t=3397
Answers to common questions: viewforum.php?f=63
and here viewforum.php?f=61
ScotY
Posts: 654
Joined: Sat Sep 23, 2017 7:57 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: none
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
Location: Honolulu, HI

Re: Recutting single point threads

Post by ScotY »

Thank you all for the information...very good to know this can be done! Modifying the wear offset seems to me to be the easiest way to go about it.
Post Reply